PSI - Issue 54

Ela Marković et al. / Procedia Structural Integrity 54 (2024) 156 – 163

159

4

Ela Markovi ć et al. / Structural Integrity Procedia 00 (2023) 000–000

Vickers value of surface hardness HV surface , the core hardness HV core , and the depth at which the hardness reaches 80% of hardness at the surface, R ht , is required to calculate the distribution of the hardness through the thickness. The following values of the mentioned parameters were taken for the purpose of simulation: HV surface = 540, HV core = 300, R ht = 4 mm. To model FGM in the specimen, elasto-plastic material parameters through the thickness of the specimen were required. Elasto-plastic material parameters include Young’s modulus and yield strength as well as Ramberg-Osgood parameters, the strength coefficient, K, and exponent, n , which describe the nonlinear material behavior after reaching the yield limit. To explore 42CrMo4 steel's mechanical properties, 20 sets of experimental data were compiled from existing literature (Basan et al. (2008); Boller and Seeger (1987); Damon et al. (2019); Thielen (1975)). Each data set included measurements of Vickers hardness, Young’s modulus, yield and tensile strength, strength coefficient, and exponent. Correlating hardness with other material properties eliminated the requirement for gradual variation in those properties when the gradual hardness distribution was known. The yield strength was estimated from hardness using nonlinear regression with the Levenberg-Marquardt algorithm with data from earlier mentioned sources (Eq. 3). Given that the problem involved FGM material, it was necessary to define a multilinear material model for different hardness values. To accomplish this, the relationship between the strength coefficient K , and the hardness was established using a simple linear expression (Eq. 4).

32 2,2

HV

 

R



(3)

e

2

HV HV 

  

1,27

 

347,3 519,7 

(4)

4,918

339

K

HV





No such meaningful correlation could be found between Vickers hardness HV and strength exponent n, so strain hardening exponent was approximated with a constant average value of n = 0,067. 2.3. Simulation setup and boundary conditions The finite element (FE) simulation of a tensile test was conducted using the Ansys software. Due to the specimen's thin planar structure and uniform cross section, a 2-D analysis was employed, exploiting symmetry for reduced model size and computation time. The lower part of the model was fixed to prevent movement in y direction and to establish symmetry conditions, while the upper part was subjected to a displacement Δ y Figure 3 illustrates the non-zero displacement and boundary conditions of a simplified model.

Fig. 3. Boundary conditions of simplified model used in analysis. Quarter of the specimen is modeled.

To ensure accurate and reliable results from finite element analysis, a mesh convergence analysis was conducted. The model was meshed with a number of elements around the circumference of quarter of the notch selected as an optimizing parameter (ranging from 2 to 16, see Figure 4) to conduct the assessment of the mesh. Given the primary focus on the region surrounding the notch, a finer line division size was applied as the notch was approached, leading to a higher density of elements in the immediate vicinity of the notch. Number of elements on other geometry lines were correlated to the number of elements on the notch radius. For the purposes of mesh convergence study, the numerical analysis without including the material nonlinearities was performed, with a Young’s modulus of 200 GPa and Poisson’s ratio of 0,3. The upper line of the geometry was